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A Look at SOLIDWORKS Toolbox

A Look at SOLIDWORKS Toolbox

Since Cimlogic’s Toolbox was certified as a Gold Partner add-in for the release of SOLIDWORKS 1999, the add-on has seen dramatic changes, such as SOLIDWORKS’ purchase of Cimlogic’s Toolbox in 2011.

Toolbox has gone from being a library of standard components to a tool for automating and standardizing the use of purchased components, such as Fasteners. In this article, we will look at how to configure SOLIDWORKS Toolbox and maximize its use for your organization’s needs.

Toolbox is bundled with SOLIDWORKS Professional and Premium. Toolbox is an add-in, meaning it can be enabled and disabled in SOLIDWORKS from the Tools pull-down, by selecting Add-ins. There are two add-ins associated with Toolbox: the SOLIDWORKS Toolbox Library and SOLIDWORKS Toolbox Utilities.

SOLIDWORKS Add-ins.

As well as enabling the add-in, the path to the Hole Wizard/Toolbox folder can be defined in Tools>System Options.

Hole Wizard/Toolbox under System Options.

The path to the Hole Wizard/Toolbox folder is defined during the installation of SOLIDWORKS but it may be changed afterwards, if needed. For instance, if this folder is moved to a network drive.

Ideally, for a multi-user implementation, this folder should be placed on a network drive and all users should have their Hole Wizard/Toolbox pointed to this location.

For organizations that use data management packages, such as SOLIDWORKS PDM, a common network location may not be required as Hole Wizard/Toolbox can be “vaulted” and a local copy can be cached. By defining a common Hole Wizard/Toolbox, we can ensure that all users will have the same settings for Toolbox.

The SOLIDWORKS Hole Wizard and Toolbox share the same Folder, as they share some of the same reference files.

Once the add-in is enabled and the correct path defined, Toolbox components can be accessed from the Design Library tab of the SOLIDWORKS Task Panel.

Toolbox library.

The contents that are available from the Toolbox menu will depend on how Toolbox is configured. We can configure the Toolbox through Toolbox Settings. These settings can be accessed by selecting Configure from the Hole Wizard/Toolbox tab of SOLIDWORKS System Options.

Common to all Steps is the Menu bar where changes can be saved and where we can navigate between the Steps and the Home page.

Toolbox Setting Menu Bar.

Step 1:

The first Step is where we define the settings for Hole Wizard. In this Step, we can define what Standards will be available.

Hole Wizard Standards.

From within each Standard, we can define which Hole Types are available.

Hole Types.

And then define which sub-types will be available.

Hole Sub-types.

Step 2:

In the second Step, we define which Hardware, such as Bolts and Screws, will be available. This process is similar to that used when defining available Hole Wizard Holes. As with the Hole Wizard Step, we define the Standards, Component type and one or more sub-types.

Configuring Toolbox Components.

It is important to note that there are other Toolbox components aside from Bolts and Screws.

Toolbox Components.

By limiting the Hole Wizard Holes and Toolbox components, we constrain what standard components a user has access to. This can limit users to only use components that your company stocks. This can be especially useful for new employees who are not yet familiar with your organization’s processes.

Beyond limiting which Toolbox components are available, in Step 2 we can to modify the Standard Properties for these components. This includes Custom Properties, Component Numbers and Descriptions.

Toolbox Standard Properties.

In the Standard Properties section, different aspects of the Toolbox component can be controlled. In the General tab, the Description and Filename can be modified. Here we have another opportunity to specify whether or not the Toolbox component will be available.

General Standard Properties.

The tabs available will depend on the type of Toolbox component. Since Bolts and Screws are often the most commonly used, we will look at some of the tabs available to these components.

In the Size tab, we can enable or disable Sizes for the selected fastener. We can also add or delete a Size, as well as control various aspects of each Size, such as dimensional values.

Fastener Size.

Closely related to Size and containing many of the same options, is Length.

Fastener Length.

Like Size and Length, Thread Data can also be configured.

Thread Data.

As mentioned previously, the aspects that can be configured for Toolbox components will depend on the component being customized.

Custom Properties can be defined for a Toolbox component by clicking on “Add new Custom Property.”

Adding Custom Property.

Once created, a Custom Property can be added to the currently selected Toolbox component. The Custom Property can also be edited or deleted.

Applying Custom Property.

Any applied Custom Property value will be displayed for the component and in the list of Configurations.

Toolbox Component Custom Properties.

To facilitate the modification of Toolbox components, the configuration information can be exported to Excel and after all the changes have been completed, these changes can be imported into Toolbox.

Import/Export Configuration Data.

The process to Customize Hardware can be lengthy. To avoid accidental loss, Back Ups should be performed regularly.

Back-up Toolbox Settings.

Step 3:

SOLIDWORKS Toolbox can create Configurations of Toolbox components, or create new components, for each size. This occurs when a particular size is used for the first time. Defining how these sizes are created is done in Step 3, “User Settings.”

User Settings.

When Toolbox is first installed, each component contains a single configuration. These initial components are located in the Browser subfolder of the Hole Wizard\Toolbox folder. If the option to Create configurations is used, the Configurations will be added to these components.

Browser Sub-folder.

Using the option to Create Configurations may result in fewer components in your Hole Wizard\Toolbox folder, but these components can become bloated with configurations. For commonly used Toolbox Components, there can be dozens of sizes and therefore dozens of configurations. The file size of these components can be large and can significantly impact performance. Also, if your organization employs a data management system, physical components are often preferred. If you do need to use configurations, try to limit the available sizes (refer to Step 2). There are also options inside SOLIDWORKS for purging Configuration information, which may help with the size of the Toolbox Components.

The Create Parts option will create a new Toolbox component once a size is used for the first time. While this will add more components to your Toolbox folder, these components are generally smaller in file size and will likely offer better performance. This is especially true of assemblies that contain many Toolbox Components.

If Create Parts is selected, these components are created in a specified folder. By default, this folder is the CopiedParts sub-folder of the Hole Wizard\Toolbox folder.

Specifying Where to Create Toolbox Components.

The last option for how different sizes of Toolbox Components are created, is to Create Components on Ctrl-Drag. If the Toolbox components are not Ctrl-dragged (holding the Ctrl key down, while dragging the component into an assembly), a Configuration is created. This is a hybrid solution that can lead to inconsistency in your Toolbox.

By default, the Hole Wizard/Toolbox folder has the Windows Read-only Attribute set.

Read Only Attribute for Toolbox Folder.

When adding a Configuration to a Toolbox Master Component, the read-only attribute needs to be changed so that the Configuration can be added to Component. The option, “Always change read-only status of document before writing” will temporarily change this attribute.

Setting Read-Only Status.

The option, “Error when writing to a read-only document” will prevent the file from being written to and will generate an error. This is sometimes used when working with Toolbox in a PDM (Product Data Manage) environment.

“Allow duplicate component number for geometrically equal components” allows the use of the same PartNumber, for more than one Configuration of a Toolbox Component, if the Configurations are geometrically identical. This can be used when a Configuration Specific Property differs between Components that are otherwise the same.

Allowing Duplicate File Numbers.

The last section of User Settings, controls what Component Name is displayed in the FeatureManager (i.e. Filename, Configuration, Description).

Setting Display Options.

Step 4:

To control who can make changes to Toolbox Settings, a password should be created. What is permitted to be changed can also be controlled in this Step.

Setting a Password and Permisssions.

At least two people should know this password.This way, if one person is not available, another will be available to make any required changes. At the same time, the number of people that know this password, should be limited to those that understand Toolbox Settings and have been designated as Toolbox administrators.

Step 5:

Smart Fasteners can be used to automatically populate assemblies with the appropriate fasteners. The fasteners that are inserted are based on existing holes and Hole Wizard holes.

Washer sizes can be restricted to only show washers that are an Exact Match or within a given tolerance of a fastener. All washer sizes can be displayed if the Unrestricted option is chosen.

Setting Washer Filter.

If selected, “Automatic Fastener Change” will change the length of the fastener being inserted by the user-specified value for Thread Engagement. “Change Stack components when fastener size is changed” will change nut and washer sizes automatically when the fastener size changes.

SOLIDWORKS Toolbox is a powerful tool, especially when working with Standard components such as Fasteners. This is achieved through the ease of using Toolbox, while ensuring consistency as well. To get the most out of it, Toolbox needs to be configured and deployed correctly.

Joe Medeiros is a senior applications engineer at Javelin Technologies, a SOLIDWORKS reseller servicing customers throughout Canada. Joe has been involved with SOLIDWORKS since 1996. An award-winning blogger, he regularly writes about SOLIDWORKS products.